No convergence

[shenrilin]

Dear all,

I'm working on phase field method, a coupled nonlinear system.

Consider a bar problem with one end fixed and the other end applied tension load.  The displacement load curves have three forms(Load curve.png).

(1) the material is homogeneously deformed, the damage is homogeneous.  If load b is applied, it works well. If load a or c is applied, the program diverges on the transition point.

If I set a very high damage criterion, all these three loads work because the problem becomes linear elastic.

(2) a flaw is located in the center of the model to generate a damage localized spot. Even if the load b is applied, it is still diverging after several time steps.

The bar problem is simulated using 1d element and 2d, 3d element with Poisson's ratio to be 0.0.

Could anybody give me some suggestions?

Best,

[Yaakov]

Hey,

It seems that you want to define a dynamic loading and a cycle loading in FEAP, It would be better that you put input files here, perhaps there are some errors in input file.

Regards,

Yaakov

[shenrilin]

Dear Yaakov,
Thank you for your reply.

Here, I attached the input file and solve file. Please look at the file.

By the way, I want to ask how to increase the time step size after the step size is decreased because of convergence requirement. Is it self-ajustable?

Thank you very much.

[shenrilin]

Sorry, I forgot the input file in the last reply and attached it here.

[Prof. R.L. Taylor]

This input file will not help -- missing too much and requires your element.  How big is the problem?

If the 1-d bar "fails" in tension (e.g., tangent becomes very small in phase field) then convergence will be hard.  Some redundancy is needed perhaps.   Sometimes the time step can be adjusted using the AUTO time step command.  This can reduce and increase the DT value when convergence is an issue.  However, very poorly conditioned problems probably cannot be fully controlled with our method.

[Yaakov]

Hi shenrilin,

I attached the input file which we used for 1 d-bar phase-field problem (only run in FEAP, not with other solvers). It works well for 1d- bar user-element.

From Prof. Taylor's suggestion we should use the residual stiffness \eta in the model in order to avoid zero stiffness (see articles from Miehe, Kuhn & Mueller, Weinberg & Hesch ...). 0<\eta<=1.0d-4.

Some Infos about auto time command: http://feap.berkeley.edu/forum/index.php?topic=1640.0

we can define a simple cycle loading via following batch commands to check your user element at first.

Code: [Select]

batch
 prop,,1
 dt,,0.0001
end
2,3
0,0 0.5,1 1,0
Kind Regards,
Yaakov

[Yaakov]

Hi,

I have checked your input file (2 d Problem, not 1 d Problem).

Add tol,,1.0d-12 (or tol,,1.0d-9)to batch solver and use auto time command, ODER 001,  you may solve phase-field convergence problem.

in this case: the main reason for convergence problem (if there is no bug in user element):
1. large value of mobility factor
2. irrversibility condition.

you have used \eta = 0,0001 here.


Regards,
Yaakov

[shenrilin]

Dear Yaakov,

Thank you very much. I have checked your shared input file and learned much.

(1) Could you please tell me what is the mobility factor?

(2) irreversibility has been ensured by the strain energy history functional and its derivatives.

(3) My auto command is presented in the inner loop so that every time step, this command can work.
 I'm not sure the parameters I set for auto time command, Auto, 2,20,150, is reasonable.  Should I change sth?

Best,

[Yaakov]

Hi shenrilin,

you are welcome!

1. for mobility facotr (other name> 1/M Viscos parameter)see- Thermodynamically consistent phase‐field models of fracture: Variational principles and multi‐field FE implementations C Miehe, F Welschinger, M Hofacker International Journal for Numerical Methods in Engineering 83 (10), 1273-1311   
2. There are three options (method) for definition of irrversibility BC, history value of sum of energy is the third one, first and second options see articles by Kuhn und Mueller (2010) and Prof.Christian Miehe Article 2010a or some new articles by Weinberg/Hesch
3. you should use paradiso (see feap forum to get useful infos.) for phase-field problem!  This FEAP Command should be a huge help for us as it reduces the most simulation time!
you can see the example about how to use auto time command
http://feap.berkeley.edu/forum/index.php?topic=1640.0=

from your 3. question, could you  tell me the configuration of your computer (RAM, CPUs,...) and the size of FE-problem (Number of Dofs, Elements)?

Regards,
Yaakov


 

[shenrilin]

Dear Yaakov,

Thank you very much.

1) I'm not using mobility factor to stabilize my system. I looked at the paper you referred and I'm sure a reasonable molibity factor would help to converge. I would try;

2) I'm reading this papers you mentioned. I would compare these methods to find the most suitable method for me;

3) Did you mean parallel computation by "paradisco"?  I'm not sure this will work for me. In my problem, only 2000 elements are used to model a crack propagation. But the time step in my problem always becomes very small compared with its initial value, for example, dt varies from 1.0e-2 to 1.0e-9.  I'm now using linearly increasing displacement load control so that the decrease of time step means it's hard to reach the end of time. 

Thank you again for your help!

Best regards,
Rilin

[Yaakov]

Dear Rilin,

 In FEAP forum, I also got many many technical & theory supports from Prof. Taylor, Prof. Govindjee, FEAP Administrator and FEAP Users ,e.g. Dr. Li ...
 
to your question
3) yes, for 2000 elements you find almost no differences (one CPU is enough), but for large size FE problems, you will find that feap runs in many CPUS in the same time, this very important function you can find in ABAQUS 16 or Ansys 17.
(in Abaqus you can use GPUS..).

use command HTOP in terminal to find the advantages of this FEAP function.

Best regards,
Yaakov